Dimensional tolerances to ISO 286: the complete guide

Every part of a flat-pack cabinet comes out of a different factory, often in a different country, and when you put them together they fit. That is not luck: it is the result of a precise language in which design tells production how far off it may be. That language is dimensional tolerancing.

The word comes from the Latin tolerare, to bear. Tolerances are the deviations we are willing to accept without losing the function of the part. They are not mistakes: they are deliberate design decisions, and they are how a functional requirement becomes something measurable and checkable.

This guide starts from the basics, works through the whole ISO 286 system, solves five worked examples step by step, and closes with the standards, the manufacturing processes and the mistakes not to make.

1. Why tolerances exist

One idea underpins everything: the exact part does not exist. Temperature swings, tool wear, machine vibration, the operator's skill — all of it introduces deviation. All you can do is define a band of acceptability inside which the actual size must fall for the part to do its job.

Take a shaft that must turn inside a hole. If the drawing says ⌀50 for both, and the workshop delivers a shaft at 50.004 and a hole at 49.998, the shaft does not fit. Nobody made a mistake: both parts are as close to 50 as anyone could reasonably ask. The mistake is in the drawing, which never said which side of 50 mattered.

The trade-off is always the same. Tight tolerances buy accuracy but cost more to make: better machines, more passes, stricter inspection, more scrap. Loose tolerances make production fast and cheap, at the risk of assemblies that do not work. A good designer does not ask for the highest accuracy available, but for the accuracy required.

2. The minimum vocabulary

One convention to learn straight away, because it is universal in technical drawing: capitals for holes, lowercase for shafts. If you read H7 you are looking at a hole; if you read h6, a shaft.

3. How tolerances appear on the drawing

3.1 Explicit deviations

The deviations written directly next to the dimension:

This is the most direct and least ambiguous method, right for isolated dimensions or for anything that does not belong to a standard fit. Note the asymmetric case: +0.025/0 means the part may grow but must never fall below nominal. That is not a rounding convenience — it usually means something has to fit inside.

3.2 ISO tolerance classes

For mating dimensions the coded system is used: ⌀50H7 for a hole, ⌀50g6 for a shaft. The letter says where the tolerance zone sits relative to the zero line; the number says how wide it is.

3.3 General tolerances

Putting deviations on every single dimension would clutter the drawing until it became unreadable. For non-critical dimensions the general class is called up once, in the title block: General tolerances: ISO 2768-m. Every dimension without a tolerance of its own then follows that class automatically.

In daily practice: ISO classes for functional fits, explicit deviations for special dimensions, general tolerances for everything else.

4. The ISO 286 system

The system is defined by ISO 286-1, which sets out the basis, the terminology and the deviations, and by ISO 286-2, which holds the tables of values. It has two components: the tolerance grade and the position of the zone.

4.1 IT grades: how wide the zone is

There are eighteen, from IT01 to IT18. The lower the number, the tighter the tolerance. A grade is not a fixed number of millimetres: it widens with size, because holding ten micrometres on a 5 mm pin and on a 500 mm bore are not the same job.

Values in micrometres: 1 µm = 0.001 mm. Grades IT01 to IT4 are missing here because they belong to gauges and measuring instruments, not to general engineering parts; grades above IT12 cover rough processes and are listed in full in ISO 286-2.

4.2 Positions: where the zone sits

The letters place the tolerance zone relative to the zero line.

Note that holes and shafts move in opposite directions: for a shaft, the letters before h remove material and create clearance; for a hole, the letters before H add space and do the same thing. It is symmetric, but it confuses everyone the first time.

4.3 Fundamental deviations

For each position the standard gives one deviation, the one on the side of the zero line; the other follows from the IT grade. For letters a to h the tabulated value is the upper deviation es, and the lower one follows by subtracting the IT. From k onwards the tabulated value is the lower deviation ei, and the upper one follows by adding the IT.

Values for shafts, in micrometres. For holes the same figures apply with the sign reversed and the matching capital, except for positions J, K, M and N at the finer grades, where ISO 286-2 introduces a correction: those must be read from the table, not worked out in your head. Above 50 mm some positions subdivide the size ranges further — at 65 and at 100 mm, for instance — so beyond that point you consult the standard rather than extrapolate.

4.4 Hole basis or shaft basis

On a hole basis the hole stays fixed at H and the fit is changed by moving the shaft: H7/g6, H7/k6, H7/p6. On a shaft basis the shaft is fixed at h and the hole moves: F8/h7, K7/h6, P7/h6.

The first is used in the overwhelming majority of cases, and the reason is economic. A hole is produced with a reamer or a broach of a definite size, and changing its tolerance means buying a new tool; a shaft can be turned to any diameter with the tool you already have. Shaft basis earns its place when one through shaft has to mate with several different holes: then it pays to hold the shaft still and move the holes.

5. The three kinds of fit

Mating a hole with a shaft gives one of three situations.

• Clearance. The shaft is always smaller than the hole: the parts move freely. H7/g6, H8/f7, H9/d9.
• Transition. Depending on where each part falls you get slight clearance or slight interference: accurate location that can still be taken apart. H7/js6, H7/k6, H7/n6.
• Interference. The shaft is always larger than the hole: press or heat assembly, a permanent joint. H7/p6, H7/s6, H7/u6.

6. Five worked examples

Example 1 — Clearance fit: ⌀50 H7/g6

A piston sliding in a cylinder: enough clearance is needed for the oil film. Diameter 50, so the range is over 30 to 50.

1. Hole H7. From the table, IT7 = 25 µm. Position H forces EI = 0, so ES = +0.025 mm. Hole from 50.000 to 50.025 mm.
2. Shaft g6. IT6 = 16 µm; position g gives es = −9 µm, so ei = −9 − 16 = −25 µm. Shaft from 49.975 to 49.991 mm.
3. Minimum clearance = smallest hole − largest shaft = 50.000 − 49.991 = 0.009 mm.
   Maximum clearance = largest hole − smallest shaft = 50.025 − 49.975 = 0.050 mm.

The clearance stays positive throughout, between nine and fifty micrometres: every part made to that drawing slides, none seizes and none rattles.

Example 2 — Transition fit: ⌀25 H7/k6

A bearing seat: accurate location, still removable. Diameter 25, range over 18 to 30.

1. Hole H7. IT7 = 21 µm, EI = 0, ES = +0.021 mm. Hole from 25.000 to 25.021 mm.
2. Shaft k6. IT6 = 13 µm; k gives ei = +2 µm, so es = +2 + 13 = +15 µm. Shaft from 25.002 to 25.015 mm.
3. Worst case one way: smallest hole with largest shaft, 0.015 mm of interference.
   Worst case the other way: largest hole with smallest shaft, 0.019 mm of clearance.

You do not know in advance which of the two you will get — hence the name. The bearing will be located accurately and will come off with a puller.

Example 3 — Interference fit: ⌀40 H7/s6

A gear ring shrunk onto a shaft: a permanent joint. Diameter 40, range over 30 to 50.

1. Hole H7. IT7 = 25 µm. Hole from 40.000 to 40.025 mm.
2. Shaft s6. IT6 = 16 µm; s gives ei = +43 µm, so es = +43 + 16 = +59 µm. Shaft from 40.043 to 40.059 mm.
3. Minimum interference = smallest shaft − largest hole = 40.043 − 40.025 = 0.018 mm.
   Maximum interference = largest shaft − smallest hole = 40.059 − 40.000 = 0.059 mm.

The shaft is always larger than the hole: it needs a press, or the ring is heated to expand it, slipped on and left to cool. Mind the order of the terms: minimum interference comes from the combination most favourable to assembly — small shaft in large hole — not from the larger absolute number.

Example 4 — Explicit deviations: 65 +0.04 / −0.02

A functional dimension that does not belong to a standard fit, a shoulder for instance.

1. Maximum size = 65 + 0.04 = 65.04 mm; minimum = 65 − 0.02 = 64.98 mm.
2. Tolerance zone = ES − EI = 0.04 − (−0.02) = 0.06 mm, that is 60 µm.

In the 50–80 range that value falls between IT8 (46 µm) and IT9 (74 µm), so the dimension is looser than IT8 and tighter than IT9. It is straightforward turning work.

Example 5 — Shaft basis: ⌀30 F8/h7

One through shaft that has to mate with several different holes. Diameter 30 — careful, it falls in the over 18 to 30 range.

1. Shaft h7. IT7 = 21 µm; h gives es = 0, so ei = −0.021 mm. Shaft from 29.979 to 30.000 mm.
2. Hole F8. IT8 = 33 µm; position F gives EI = +20 µm, so ES = +20 + 33 = +53 µm. Hole from 30.020 to 30.053 mm.
3. Minimum clearance = 30.020 − 30.000 = 0.020 mm.
   Maximum clearance = 30.053 − 29.979 = 0.074 mm.

The shaft is the reference and the hole provides the clearance. To mate the same shaft with another component you simply change the hole position: G8, H8, and so on.

7. General tolerances to ISO 2768

For non-critical dimensions ISO 2768-1 defines four classes of accuracy, called up once in the title block.

7.1 Linear dimensions

7.2 Angular dimensions

7.3 General geometrical tolerances

ISO 2768-2 covers geometry with classes H, K and L. Straightness and flatness depend on the length of the feature; they are not a single value:

Perpendicularity and symmetry also depend on the length of the side; circular run-out, by contrast, is a single value per class: 0.1 for H, 0.2 for K, 0.5 for L.

Choosing the class: f for precision engineering, m for general engineering — the right answer in the great majority of cases — c for fabrication and sheet metal, v for castings and rough parts. A drawing marked ISO 2768-mK has covered linear and geometric in six characters.

Read that in reverse and you have the discipline the standard is really teaching: if a dimension carries its own tolerance, it is because something depends on it. A drawing where every dimension is toleranced individually is a drawing whose author had not decided what mattered.

8. The standards

9. What accuracy each process gives

Every process reaches a characteristic band of IT grades. Knowing it is the only way to specify tolerances that can actually be met.

Hence the question worth asking before writing a tolerance: which process will the workshop use? Asking for IT5 on a sand casting is asking for the impossible; writing IT12 on a precision shaft means wasting the grinding operation that will be carried out anyway.

10. Common mistakes

• Tightening everything "to be safe". By far the most expensive mistake. Each IT grade can multiply the cost of the part by two or three, and on dimensions with no function that money is simply thrown away.
• Reading the wrong size range. ⌀30 sits in "over 18 up to 30". This error leaves no trace: it produces believable numbers.
• Tolerancing auxiliary dimensions. Dimensions in brackets are for information: a tolerance on them creates ambiguity and contradicts the real dimensions.
• Dimensioning the same feature twice. From two directions the part can satisfy one dimension and violate the other, and neither is wrong on its own.
• Chaining dimensions. Tolerances add up: four features at ±0.1 in a row can put the last face 0.4 mm from nominal. If the stack matters, dimension from a single datum.
• Specifying tolerances nobody can measure. If the workshop has no instrument to check it, the tolerance does not exist: it exists only on paper.
• Applying a fit code to a feature that fits nothing. H7 on a clearance hole for an M8 screw is not precision: it is expense with no purpose.

11. In short

• Specify the accuracy required, not the highest available.
• Use hole basis where you can: it is cheaper.
• For non-critical dimensions, rely on the general tolerance in the title block.
• Always check that the tolerance can be measured with the instruments that exist.
• Account for accumulation in dimension chains.
• Remember the convention: capitals for holes, lowercase for shafts.
• On drawings from elsewhere, check whether ISO or ASME rules apply.

Tolerances are rather like traffic rules: they look as though they restrict freedom, and in fact they are what makes it possible. Without them every part would go its own way and no assembly would stand up.

12. Putting it on a sheet

Reading only takes you so far. Take a sheet from the archive with a shaft and a housing, decide for yourself which dimensions are functional, choose fits for those and a general class for everything else, and write it on the drawing. Then change your mind about one fit and see how far the consequences travel.

That last step is the one that teaches. A tolerance is never a property of a single feature: it is a statement about a relationship, and relationships are where drawings get interesting.

The next article in the series will take on geometrical tolerancing to ISO 1101: what happens when size alone is not enough to describe what a part has to do.